Was going to give the new Structure System a test, and none of the weldment profiles show up. The "standard" list populates as should, but "type" and "size" doesn't pull anything from the folders. Working just fine in weldments.
You need a configured weldment library. The default library isn't. How to create a configured weldment profile is mentioned in the weldment training material. I believe there is a download with a configured library. The new 2019 library is configured by default.
S-075348 When I create a structure system in the SOLIDWORKS® software, why are my weldment profiles unavailable?
Structure systems use only configured profiles.
In previous SOLIDWORKS® versions, the sample weldment profiles each contained one configuration. The folder structure of the weldment profile directory determined the standard, type, and size of each profile. In this setup, each SLDLFP file represented a size.
In the SOLIDWORKS 2014 version, it became possible to add multiple configurations to a weldment profile.
Effective with the release of SOLIDWORKS 2019, the sample weldment profiles each contain multiple configurations. The folder structure of the weldment profile directory determines the standard and type. In this setup, each SLDLFP file represents a type and contains multiple sizes.
Structure systems require the latter setup in which the folder structure determines the standard and type and the configuration determines the size.
To convert custom weldment profiles to the newer format:
1. Edit the SLDLFP file and add a configuration for each size.
2. Configure the sketch dimensions as necessary.
3. In Windows® Explorer, move the SLDLFP file up one level to the folder for the standard.
Structure systems are available effective with the SOLIDWORKS 2019 version.
It doesn't seem to have installed any configured weldments. Where would I be able to download the 2019 samples?
It should be in C:\Program Files\SOLIDWORKS CORP\SOLIDWORKS\lang\english\weldment profiles (the ansi inch.zip)
Thank you for uploading the Configured Weldment Profiles.
How did you got it from Solidworks or you make it by yourself?
I got one from SolidWorks, the other from the installation of 2019.
your configured profile has all the ansi profiles but for ISO there are only few profiles.
Hi Ruban Antony,
I never reviewed the content myself, but I believe you are right.
Depending on the type you are missing, dimensions can be (easily) added as the profiles are "configured". But I think T-section would need some sketching. I think a weldment library should be personal, i.e. not all dimensions of the profiles mentioned in the Standard are available on the market or lying around on your shop floor.Kind regards,
i'm a solidworks trainer, i need to show the trainees that solidworks supports all standards. i'm okay with weldments, but since this structure system is new i'm having few troubles, as you said no one needs all profiles since they can customize it according to their needs, but any student would have same question as mine, and that would e why structure system doesn't show any of the downloaded profiles while weldments does? and i'm also aware that structure system shows only configured items. is there any other way to show all the downloaded profiles in structure system?
I have the same problem aswell, the thing is i don't have any zip files in the solidworks installation file, so i downloaded the profiles from solidworks content tab, since i need it for training purpose i want all profile standards and so downloaded all of them, but as kyle said the profiles are not showing in structure system but works fine in the weldments.
There seems to be more going on that just having configurations in the profiles. When configurations became available for weldment profiles a few years ago, I played around with that and it worked nicely. But those same configured profiles in Structure Systems are not recognized. After the first pull-down, the Type and size menus are empty...
Something else must be needed for them to work in Structure Systems that isn't explained in the help and What'sNew 2019 documentation. I must be missing some little detail, but I can't figure it out.
Has anybody else experienced this same problem with custom configured profiles?
Your folders must not be structured correctly, nothing special needs to be done to the profiles.
..../weldment profiles/(folder name)/profile.sldflp
If you have a second sub folder like the old weldments (...weldment profiles/iso/c channel/profile.sldflp) then the parts won't be recognized.
Maybe drop one of your profiles here if that doesn't help
Thanks, Kyle, but I do have the correct folder structure (for several years). All my standard and custom profiles work in weldments, but not structure systems.
I think I have to re-examine the configurations. Looking at the 2019 profiles that do work in structure systems, I see something slightly different in the configuration manager. There is a table, not a design table, but it isn't.
In my custom configured profile library files, I don't see the table.
Everything else looks the same. I have a feature (sketch) in the Feature Manager selected as a library item, and I added the "Profile Properties" folder to the Feature Manager.
Okay I see the problem. While you do have configurations, the structure system reads information from design tables, not just configurations. Open up your profiles and go to "instert->tables->design table"
If you're not familiar with how those work you definitely should read up on them. If you do, then you'll be good to go. It should have no issues translating over the configurations you have already made into the correct columns and rows in the spreadsheet. This is also a much easier way to add configurations
that is NOT a design table in his screenshot....
Okay you're right, but a design table is the preferred method. If you want THAT table, which I prefer not to use... just follow these steps.
Right click on any feature of your part and click "configure feature"
It will bring up a table window. Where you see "<Enter Name>" just type in "table" or whatever you want to name it.
Then to the left of that you can save it. It will show up under the tables in the configurations tab like that part.
But, like I said, you should use design tables. It's super easy to add and modify configurations using those, and all of the other structural weldments SW has are done with this method. If you don't have those, the link is up the thread posted by Richard Bremmer
Thanks, Kyle, I never paid attention to naming the "configure feature" tables before. I suspected it was something simple like that though.
My preference is also design tables - been doing really large and involved ones for years to build entire part libraries with rules and all to guide users on creating new valid configurations. My profiles are far simpler and maybe don't need something as sophisticated as a design table.
Correct, Jeremiah. That's the weird part about it. How did that non-design table get there?
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